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Swept Cut PropertyManager

Set the PropertyManager options based on the sweep cut feature.

To open this PropertyManager:

  1. Open a part that has either a closed profile sketch and a sketch path, or a part with a sketch line, edge or curve on the model that you can specify as a path.

    For a solid profile, open a part that has a tool body as the profile and a sketch path to follow.

  2. Click Swept Cut (Features toolbar).

Sketch Profile

Creates a sweep by moving a 2D profile along a 2D or 3D sketch path.

Profile Sets the profile (section) used to create the sweep. Select the profile in the graphics area or FeatureManager design tree. The profile must be closed for a base or boss sweep feature. The profile may be open or closed for a surface sweep feature.
Path Sets the path along which the profile sweeps. Select the path in the graphics area or FeatureManager design tree. The path can be open or closed, and can be a set of sketched curves contained in one sketch, a curve, or a set of model edges. The start point of the path must lie on the plane of the profile.

The following controls are available when the path extends through a profile.

Direction 1 Creates a sweep for one side of the path.
Bidirectional Creates a sweep that extends in both directions of the path from a sketch profile.
You cannot use guide curves or set the start and send tangency for a bidirectional sweep.
Direction 2 Creates a sweep for the other direction of the path.
You can control the twist value of the path independently for each direction of the sweep and apply the twist value over the entire length.

Circular Profile

Creates a solid rod or hollow tube along a sketch line, edge, or curve directly on a model.

Profile Sets the profile (section) used to create the sweep. Select the profile in the graphics area or FeatureManager design tree.
  Diameter Specifies the diameter of the profile.
   
Neither the section, the path, nor the resulting solid can be self-intersecting.

Solid Profile

The most common usage is in creating cuts around cylindrical bodies. This option would also be useful for end mill simulation.

When you select Solid Sweep, the path must be tangent within itself (no sharp corners) and begin at a point on or within the tool body profile.

Solid profiles are not available for assembly features.

Tool Body The tool body must be convex, not merged with the main body, and consist of one of the following:
  • A revolved feature that consists of analytical geometry only, such as lines and arcs.
  • A cylindrical extruded feature.
Path Sets the path along which the profile sweeps. Select the path in the graphics area or FeatureManager design tree. The path can be open or closed, and can be a set of sketched curves contained in one sketch, a curve, or a set of model edges. The start point of the path must lie on the plane of the profile.
   
Tool body and path
Cut sweep

Note how Solid Sweep handles a tool body following a helix path.

Guide Curves

Only applicable for sketch profiles. However, they are not bidirectional sweeps.

Guide Curves Guides the profile as it sweeps along the path. Select guide curves in the graphics area.
The guide curve must be coincident with the profile or with a point in the profile sketch.
Move Up and Move Down Adjusts the order of the guide curves. Select a Guide Curve and adjust the profile order.
  Merge Smooth Faces Clear to improve performance of sweeps with guide curves and to segment the sweep at all points where the guide curve or path is not curvature continuous. Consequently, the lines and arcs in the guide curves are more accurately matched.
   
Merge Smooth Faces selected
Merge Smooth Faces cleared
When you clear Merge Smooth Faces, the potential exists that some features created later might fail due to the changed geometry.
Show Sections Displays the sections of the sweep. Select the arrows to view and troubleshoot the profile by Section Number.
   

Options

  Profile Orientation Controls the orientation of the Profile as it sweeps along the Path .
   

Follow Path

Section remains at same angle with respect to path at all times.

When you select Follow Path, options stabilize the profiles when small and uneven curvature fluctuations along the path cause the profiles to misalign.

Keep Normal Constant

Section remains parallel to the beginning section at all times.

If there are multiple profiles, sections remain parallel to the beginning section at all times.

  Profile Twist Applies twist along the path. Select one of the following:

None

(For 2D paths only.) Aligns the profile normal to the path. No correction is applied.

Minimum Twist

(For 3D paths only.) Prevents the profile from becoming self-intersecting as it follows the path.

Follow Path and First Guide Curve





Select Follow Path and First Guide Curve and the twist of the intermediate sections is determined by the vector from the path to the first guide curve. The angle between the horizontal plane and the vector remains constant in the sketch planes of all of the intermediate sections.

Follow First and Second Guide Curves



Select Follow First and Second Guide Curves and the twist of the intermediate section is determined by the vector from the first to the second guide curve. The angle between the horizontal plane and the vector remains constant in the sketch planes of all of the intermediate sections.

Specify Twist Angle

Define the twist of the profile along the path. Select Degrees, Radians, or Revolutions.



This example shows one turn.

Twist Along Path With Normal Constant

Twists the section along the path, keeping the section parallel to the beginning section as it twists along the path.



This example shows one turn.

Specify Direction Vector

Select a plane, planar face, line, edge, cylinder, axis, a pair of vertices on a feature, and so on to set the direction vector. Not available with Keep Normal Constant.

Tangent to Adjacent Faces

Available when attaching a sweep to existing geometry. Makes the adjacent faces tangent at the profile.

Natural

(For 3D paths only.) As the profile sweeps along the path, it pivots to maintain the same angle relative to the curvature in the path.

  Merge Tangent Faces If the sweep profile has tangent segments, causes the corresponding surfaces in the resulting sweep to be tangent. Faces that can be represented as a plane, cylinder, or cone are maintained. Other adjacent faces are merged, and the profiles are approximated. Sketch arcs may be converted to splines.
  Show Preview Displays a shaded preview of the sweep. Clear to display only the profile and path.

Examples for solid sweeps:

When you select Follow Path for the Orientation/Twist Type, and None for Path Alignment type, the tool body correctly follows the tangents of the helix path.



To keep the tool body perpendicular to a reference as it follows a helix path, select Direction Vector for Path Alignment Type, then select a direction to which the tool body remains perpendicular, for example, the normal to the planar end face of a cylinder.

The tool body remains parallel to the end face as it follows the helix path along the cylinder. This functionality is important for the tool machining market.

Start and End Tangency

Start Tangency Type and End Tangency Type.

None No tangency is applied.
Path Tangent Create the sweep normal to the path at the start.

Feature Scope

Specifies which bodies or components you want the feature to affect.
  • For multibody parts, see Feature Scope in Multibody Parts.
  • For assemblies, see Feature Scope in Assemblies.

Curvature Display

Mesh Preview Applies a preview mesh on the selected faces to better visualize the surfaces.
Mesh Density Available when you select Mesh Preview.

Adjusts the number of lines of the mesh.

Zebra Stripes Displays zebra stripes, to make it easier to see surface wrinkles or defects.
Curvature Combs Activates the display of curvature combs.

Select at least one of these options:

Direction 1

Toggle the display of curvature combs along Direction 1.

Direction 2

Toggle the display of curvature combs along Direction 2.

For either direction, select Edit Color to modify the comb color.

Scale

Adjusts the size of the curvature combs.

Density

Adjusts the number of lines of the curvature combs display.



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